Drucker–Prager Triaxial Test

3 min read • 593 words

This example simulates a conventional triaxial compression test using the Drucker–Prager model in a single 8-node brick element. Stress and strain response are recorded at the Gauss point.

On this page

Python Tcl

drucker.py

drucker.tcl

This model simulates the triaxial compression behavior of a soil-like material subject to confining pressure and axial loading. The simulation is conducted using a single 8-node stdBrick element with Drucker–Prager plasticity . The goal is to evaluate material behavior under both hydrostatic and deviatoric loading paths.

Model

We begin by defining the model builder and creating the nodes of the brick:

import xara model = xara.Model(ndm=3, ndf=3)

model.node(1, (1.0, 0.0, 0.0)) model.node(2, (1.0, 1.0, 0.0)) model.node(3, (0.0, 1.0, 0.0)) model.node(4, (0.0, 0.0, 0.0)) model.node(5, (1.0, 0.0, 1.0)) model.node(6, (1.0, 1.0, 1.0)) model.node(7, (0.0, 1.0, 1.0)) model.node(8, (0.0, 0.0, 1.0))

model BasicBuilder -ndm 3 -ndf 3

node 1 1.0 0.0 0.0
node 2 1.0 1.0 0.0
node 3 0.0 1.0 0.0
node 4 0.0 0.0 0.0
node 5 1.0 0.0 1.0
node 6 1.0 1.0 1.0
node 7 0.0 1.0 1.0
node 8 0.0 0.0 1.0

The boundary conditions are applied to simulate triaxial constraints, fixing displacements appropriately on different node sets:

fix 1 0 1 1
fix 2 0 0 1
fix 3 1 0 1
fix 4 1 1 1
fix 5 0 1 0
fix 6 0 0 0
fix 7 1 0 0
fix 8 1 1 0

The Drucker–Prager material is defined with specified parameters for elasticity, yield surface, and hardening behavior:

model.nDMaterial("DruckerPrager", 2,
    K       = 27777.78 ,
    G       =  9259.26 ,
    Fy      =     5.0  ,
    Rvol    =     0.398,
    Rbar    =     0.398,
    Fs      =     0.0  ,
    Fo      =     0.0  ,
    Hsat    =     0.0  ,
    H       =     0.0  ,
    theta   =     1.0  ,
    delta2  =     0.0  ,
    density =   1.7
)

nDMaterial DruckerPrager 2 \
   -K      27777.78  \
   -G       9259.26  \
   -Fy         5.0   \
   -Rvol       0.398 \
   -Rbar       0.398 \
   -Fs         0.0   \
   -Fo         0.0   \
   -Hsat       0.0   \
   -H          0.0   \
   -theta      1.0   \
   -delta2     0.0   \
   -density    1.7

The model includes a single stdBrick element to represent the soil specimen:

element stdBrick 1 1 2 3 4 5 6 7 8 2 0.0 0.0 0.0

Recorders

Nodal displacements and Gauss point quantities such as stress, strain, and material state variables are recorded:

set step 0.1

recorder Node -file out/displacements1.out -time -dT $step -nodeRange 1 8 -dof 1 2 3 disp

recorder Element -ele 1 -time -file out/stress1.out  -dT $step material 2 stress
recorder Element -ele 1 -time -file out/strain1.out  -dT $step material 2 strain
recorder Element -ele 1 -time -file out/state1.out   -dT $step material 2 state

Loading

Two loading patterns are defined: the first applies hydrostatic pressure, and the second imposes axial deviatoric stress:

set p 10.0
set pNode [expr -$p * 0.25]

pattern Plain 1 {Series -time {0 10 100} -values {0 1 1} -factor 1} {
    load 1  $pNode    0.0 0.0
    load 2  $pNode $pNode 0.0
    load 3     0.0 $pNode 0.0
    load 5  $pNode    0.0 0.0
    load 6  $pNode $pNode 0.0
    load 7     0.0 $pNode 0.0
}

pattern Plain 2 {Series -time {0 10 100} -values {0 1 5} -factor 1} {
    load 5  0.0 0.0 $pNode
    load 6  0.0 0.0 $pNode
    load 7  0.0 0.0 $pNode
    load 8  0.0 0.0 $pNode
}

Analysis

The analysis uses standard OpenSees commands to control the solution procedure and apply the loads incrementally:

integrator LoadControl 0.1
numberer RCM
system SparseGeneral
constraints Transformation
test NormDispIncr 1e-5 1 1
algorithm Newton
analysis Static

puts "starting the hydrostatic analysis..."
set startT [clock seconds]
analyze 1000
set endT [clock seconds]

puts "triaxial shear application finished..., [getTime]"

The output of the simulation should look as follows:

The displacements over time are:

Rigid Offsets

010 - Nonlinear torsion

On this page: